(1). When you say free jet simulation, you are simulating the real free jet problem. (2). In this case, you need to define your real free jet problem boundary condition first. That is to say, in real world test condition, how are you going to create this free jet and be able to measure the flow properties? (3). If you are not trying to simulate it, then you can put any boundary conditions there (anywhere). Hint: if you create a free jet in a test cell, you must have test cell walls, a nozzle which will create the jet, downstream exit connected to exhaust devices. In this example, the wall will be the boundary condition and the exit can be downstream condition or pressure condition depends on how you handle your jet initial(inlet) condition. (4).Try to think in terms of the real world test condition because the next step you are going to do is to perform the testing to validate your results. If your free jet is in outdoor environment, you may have to consider the wind condition.

It is a very difficult problem if you are trying to get very good result. However, it might be fairly simple if you want to know the TREND only or you can be satisfying for qualitatively(not quantitatively) consistent solution.

If you have a commercial package, for example, it is very simple to solve the problem itself. You only give pressure boundary condition for all boundaries except inlet(maybe it is a nozzle). The solution will show the amount of entrainment flow, whether the flow is leaving the domain or entering the domain and so on. I have an experience for solving free swirling flow with a commercial package. I could obtain well converged solution and it showed the trend fairly well. But I did not try to compare the result to experimental data, so that I could not discuss the accuracy.

I am working on a similar problem. I use characteristic boundary conditions for both inflow and outflow. For a 2D problem, the characteristic boundary conditions include two Riemann invariants, entropy, and parallel velocity. Now I am testing these conditions. The charateristic approach is really a "standard" one. Does anybody know a better approach particurlarly suitable for jet flow?

(1). The inlet boundary condition is fine, you can specify U and V there. (2). The exit condition is fine, you can specify zero-gradient there as long as it is far down stream. ( V can be zero there.) (3).From the jet exit (x=0), there must be a wall form r=rjet to r=router_boundary. You can specify a wall there or specify U=0 and V=0 there. Unless there is another outer stream there. In a free jet , you don't have an outer stream. This one is missing from your boundary condition. (4). The outer boundary condition is up to you to select either a wall or a far-field condition. A wall boundary condition is easier to specify. All you need to do is to set U=0, and V=0 there. If you use a wall, then a recirculating flow will be created between the jet and the outer boundary wall. This automatically provides the proper condition at the edge of the jet for you as part of the result, as long as the wall is at a large distance away from the jet. You can also use other types of conditions there. But then you have to do some reading. (5). I am assuming that you are solving the Navier-Stokes equations. Once you have the solution using this types of boundary conditions, you should be ready to use more advanced types of boundary condiitons on your own (if you don't want to place a farfield wall there). By the way, the boundary condition also depends on your formulation, whether it is a primitive variable approach, pressure-based, or a simple vorticity-stream function formulation. (if r=D/2 is your jet radius, then replace it by the outer-wall boundary condition at r=router_boundary mentioned above)

(1) rv=const. usually works for swiring flow if 'v' means swirling velocity. It's physical meaning is 'angular momentum conservation'. But it has no physical meaning if 'v' is radial velocity.

(2) If 'D' means nozzle diameter, your domain is too small to calculate entrainment from the atmosphere. If 'D' is large diameter which represents your calculation domain, how can you give the boundary condition at the region from the d/2 to D/2, the region of strong entrainment(d means nozzle diameter) ? Furtheremore, u=0 can be applicable if and only if D means far from nozzle axis, say couple of tens times of nozzle diameter.

(3) So, I think that the only possible approach is to give pressure boundary condition if you do not have experimental data for every boundary.

(1). I am surprized that most people ask questions here tend to express it as though they are classical 19 century Chinese ladies. (2). Don't try to link the question to your personality or identity. A question has to be well defined to receive an answer. And the reason why a question was answered, is because it would benefit the rest of the readers.